翻译原文.pdf

58Major Concepts of Geometric Dimensioning and TolerancingMajor Concepts of Geometric Dimensioning and Tolerancing-Converting from +to Geometric Tolerancing-Position-Gaging-Flatness-Selecting Datum Features-Perpendicularity-Mating Part Tolerancing-Reading the Feature Control Frames as a Language-Calculating Inner and Outer BoundariesVirtual ConditionResultant Condition-MMC vs. RFS vs. LMCWhat they meanWhen to use themBoundaries they createBonus Tolerancing Formulas . for Position, Perpendicularity, Angularity and Parallelism Modified at MMCAllowed vs. Actual Deviation from True Position A Difference between Bonus Tolerance (growth) and Datum feature shift(movement) of Tolerance ZonesChapter 5Downloaded From: / on 04/11/2014 Terms of Use: /terms59Chapter FiveChapter ObjectivesReaders will learn:1. How to convert from plus and minus tolerancing to geometric tolerancing.2. When Position Tolerancing applies, its tolerance zones and the boundaries it creates.3. How to select, define and tolerance datum features.4. How size controls form.5. How to measure MMC and LMC.6. How to apply geometric tolerances of flatness, perpendicularity and position in sequence. 7. The tolerance zone configuration for flatness and varieties of perpendicularity.8. How to calculate and distribute mating part tolerances.9. Practical Absolute Functional Gage design, dimensioning and tolerancing.10. How to calculate bonus tolerance for position, perpendicularity, angularity and parallelism when modified at MMC.11. The difference between using MMC symbology after geometric tolerances (tolerance zone growth) and MMB symbology after datum features (datum feature shift).12. How to calculate when a feature complies with its position tolerance and when it does not (variables data collection and analysis using CMM type data).13. How to use charts for inches or millimeters to determine position tolerance compliance.14. The meaning of Actual Mating Envelope and Actual Mating Size (both oriented and/or located vs. unoriented, unlocated) for tolerance compliance.15. How to use gages to help understand geometric controls and use of maximum material condition and maximum material boundary symbols.Downloaded From: / on 04/11/2014 Terms of Use: /terms60Major Concepts of Geometric Dimensioning and TolerancingThere are many situations where all four geometric contributors of size, shape, angle and location must be controlled. The only geometric characteristic symbols capable of tolerancing all four are in the profile category, most commonly, profile of a surface (which will be discussed in-depth later). But, if we give a regular feature of size like a simple cylindrical hole a size tolerance, the size limits will control size and form. We can then go about controlling angles and location.On the following mating parts (Part #1 and Part #2), location has been accomplished with plus and minus toleranced dimensions.FIGURE 5-1 Major Concepts of Geometric Dimensioning and TolerancingDownloaded From: / on 04/11/2014 Terms of Use: /terms61Chapter FiveFIGURE 5-2 a & b Part #1 and Part #2Downloaded From: / on 04/11/2014 Terms of Use: /terms62Major Concepts of Geometric Dimensioning and TolerancingFIGURE 5-3The angles on the part depicted here as 90 angles have been toleranced by a general tolerance note in the “unless otherwise specified” block. Unfortunately, the type of tolerancing to control the tolerances of the relationship for location between the hole on Part #1 (as well as the shaft on Part #2) and the edges of the part is ambiguous and, therefore, insufficient. For example, depending on which features are interpreted as the origin of measurement, the tolerance zones applied to the part could be quite different. If the edges of Part #1 are seen to be the implied datum features (origins of measurement), the tolerance zone for the holes location will appear as a square zone (2D) or parallelepipedic zone (3D) that may be 1mm by 1mm. This zone would be seen as measured from planes formed by the part surface high points. Its center would be 200 millimeters from one of these planes and 200 millimeters from another and perpendicular to another to complete our 3 dimensional, 3 plane coordinate system.Downloaded From: / on 04/11/2014 Terms of Use: /terms63Chapter FiveFIGURE 5-4 Unfortunately, we would only be guessing at what would be the implied primary datum feature, the secondary datum feature and the tertiary (third) datum feature in this datum reference frame (coordinate system). This is important since the person setting up and measuring the part would be required to know. They could give the primary datum feature a proper seat of a minimum contact of 3 high points of contact on the primary datum plane (simulated somehow in the measurement procedure). The secondary datum feature would get a minimum of 2 points of high point contact and the tertiary would get a minimum of 1 point of high point contact. Since no datum features are specified on the part drawing, no set up of the part would be repeatable and, therefore, no measurement data would be repeatable. Add to that the fact that another inspector might simply interpret the drawing less as a position control (which this first interpretation assumes) and more as a profile of a surface-type control. Instead of the hole measured from the edges of the part, it might be interpreted as the edges of the part are measured from the hole (which would then be assumed to be the implied datum feature). The edges of the part would be given the tolerance of plus or minus 0.5 millimeters centered on the 200 millimeter dimensions to the edges.One Possible Interpretation of Part #1Downloaded From: / on 04/11/2014 Terms of Use: /terms64Major Concepts of Geometric Dimensioning and TolerancingFIGURE 5-5This interpretation would not only locate the surfaces from the hole axis, but would (if interpreted as an implied profile of a surface control) hold a form (flatness) and angle (perpendicularity) control on the surfaces. All this is, of course, idle speculation, since the drawing has no specific true interpretation. It is poorly toleranced, ambiguous, and badly in need of improvement.Correcting the Geometric Definition and Its Tolerancing SchemeStep 1 This improvement starts off with the assignment of datum features. The primary datum feature on each part should be:1) the seating surfaces,2) the surfaces that need the most physical contact in the assembly, and3) the surfaces that dictate the angle at which these two parts will assemble.The answer to this selection can be seen in an assembly view of the side view of both parts as follows:Downloaded From: / on 04/11/2014 Terms of Use: /terms65Chapter FiveFIGURE 5-6FIGURE 5-7Therefore, the primary datum features are assigned to both parts.Downloaded From: / on 04/11/2014 Terms of Use: /terms66Major Concepts of Geometric Dimensioning and TolerancingThe only letters not used as datum features are I, O and Q. They look too much like numbers. Also, the order of the letters as they are used in the alphabet is unimportant. The only thing of importance is how these datum features will be used (referenced) in the feature control frames (geometric tolerances) on the parts.We must dwell on these primary datum features and ask the question, “What characteristic of geometry must each have to seat in the assembly without rocking too much?” Since this will be the first control assigned to each part, it cannot be a relationship control. This feature establishes the primary datum feature on each part. It is first; therefore, there is nothing to relate it to. So, it cant be perpendicular or parallel to anything because at this stage of the definition, there is nothing to relate it to. It is first. All we can do is give it a form tolerance. Since the entire surface on each part seats on the entire surface of the other part, this control must apply to the entire surface. It must be a surface control (3D), not a line element control (2D) like straightness. Since the surface has a planar shape, it must be controlled by flatness. Rule #1 says the size tolerance given to the width of the part in the side view already controls the flatness, straightness and parallelism of both sides. On Part #1, the size tolerance is 7560.03. On Part #2, the size tolerance is 100 +0.03. Rule #1 says they must each have perfect form if they are produced at MMC (75.03 for Part #1 and 100.03 for Part #2). Only as they depart from the MMC, may they depart from perfect form. For example, on Part #1 the size is verified with a simulation of a GO gage at MMC and at cross sections at LMC. A GO gage could be two parallel rails at 75.03 apart as shown in FIGURE 5-8.FIGURE 5-8 GO GageIf the part is produced at 75.03 at all cross-sectional measurements, the only way it would (even in theory) fit the GO gage is if it has perfect flatness, straightness and parallelism. But, if the part was produced smaller than 75.03 (MMC), it could be less than perfect in its form by its departure from MMC. Since the LMC of 74.97 is the smallest the part may be and still comply with the size tolerance, the most it can depart from the MMC of 75.03 is 0.06. So, even without a flatness feature control frame, the flatness is controlled by Rule #1 to within 0.06. Any Downloaded From: / on 04/11/2014 Terms of Use: /terms67Chapter Fiveadditional flatness control would have to refine (be smaller than) the 0.06 tolerance. Otherwise, it would be meaningless, since the size tolerance would control flatness better. In this case, due to cost, manufacturing capability and functional requirements, the flatness (tolerance) has been assigned as 0.01. For example:FIGURE 5-9Step 1Since both parts, when seated on one another, will dictate how much they might rock when assembled, and the parts are the same size, a flatness tolerance of 0.01 is also assigned to primary datum feature D on Part #2. What we do on one part is commonly done on the mating part. Step 2 makes us choose between the hole and the part edges as the origin of measurement. For this example, we will choose the edges. Step 2The secondary datum features on each part will be one of the two sides of the part from which the 200mm dimensions originate. The longer side would, having more surface area, lend more to part stability. The top edge in the front view of both parts is 429-431 millimeters long, about 20 millimeters longer than the left edge (the other candidate). So, the top edge will become the secondary datum feature on both Part #1 and Part #2. It is important that we choose the same edge on both parts, if possible, since we will be aligning these edges during assembly.FIGURE 5-10Downloaded From: / on 04/11/2014 Terms of Use: /terms68Major Concepts of Geometric Dimensioning and TolerancingEach of these surfaces labeled datum feature B and datum feature E will need a dimension that is basic (a boxed 200mm dimension) originating at the datum plane (constructed by a minimum of 2 high points of contact on the datum feature surface) and leading us to the hole axis. This basic 200mm dimension will be a target for manufacturing to shoot for. The tolerance, instead of being plus or minus 0.5 on the 200mm dimension, will instead be calculated in Step 4 as a position tolerance that will allow the axis of the hole on Part #1 and the shaft on Part #2 to deviate from the perfect location represented by the 200mm dimensions from the (datum planes formed by the) parts edges. These edges, which are secondary datum features (and in Step 3, tertiary datum features), must be related with a tolerance back to the primary datum. The relationship depicted between the secondary surface and the primary plane on each part is one of 90 or perpendicularity. We could simply allow the general tolerance note of 61 to tolerance this angle, but in this case, we will apply a more uniform tolerance zone of perpendicularity. It will form 2 parallel planes 0.03 apart. Both planes will be 90 to the primary datum plane (formed by a minimum of 3 high points of contact from the primary datum feature). If the surface is in the tolerance zone, it will be perpendicular to within 0.03mm and it will be flat to within 0.03mm.FIGURE 5-11 Step 2Downloaded From: / on 04/11/2014 Terms of Use: /terms69Chapter FiveOn Part #1, the tolerance zone would appear as follows in the side view:FIGURE 5-12Step 3Step #3 is to assign the remaining surface from which the other 200 millimeter dimension originates as the tertiary datum feature and to relate it to within a tolerance back to the primary and secondary datum planes. The tolerance of perpendicularity of 0.03 in Step #2 was 3 times the tolerance of flatness on the primary datum feature in Step #1 of 0.01. It is common to increase the tolerances on features to be greater than tolerances on features from which they are measured. So, if datum feature A has a tolerance of 0.01, then for measurement repeatability, we would like the tolerance on datum feature B to be greater. In this case, 3 times greater is 0.03. Sometimes, for reasons of cost, manufacturing capability or simply by being overridden by a formula for calculating mating part tolerances, this is not feasible. But, when no such condition exists, a good rule of thumb is that the tolerances given to the features from which we measure (such as the primary datum feature which constructs the primary datum plane) should be tighter than that on features being measured from them (such as the secondary datum feature B in this case).This same rule of thumb would apply to the tertiary datum features on both Part #1 and Part #2. We prefer their tolerances to be greater than those given to the secondary datum features which form the planes to which the tertiary datum features will be related. Since the tertiary datum features are depicted perpendicular (90) to both the primary and secondary datum features on both Part #1 and Part #2, the tertiary datum features will be given a perpendicularity tolerance 3 times greater than 0.03. They appear as follows:Downloaded From: / on 04/11/2014 Terms of Use: /terms70Major Concepts of Geometric Dimensioning and TolerancingFIGURE 5-13The tolerance zones for Step #3 would be two parallel planes 0.09 apart, between which must reside all points on the tertiary datum feature surface. This zone is perpendicular to both the primary and secondary datum planes. On Part #1, the zone would be as follows:FIGURE 5-14 Step 3, Part 1 tolerance zoneDownloaded From: / on 04/11/2014 Terms of Use: /terms71Chapter FiveAs it was done on Step #2, Step #3 also makes certain that the 200 mm dimension is made a basic dimension by placing a box around it and transferring the tolerance (once it is recalculated) into the feature control frame (geometric tolerance) on Step 4.Step 4Now that all 3 datum features have been assigned and toleranced, it is time to relate the hole to the 3 mutually perpendicular planes that form the datum reference frame (coordinate system) on Part #1. Likewise, the shaft on Part #2 will be geometrically toleranced to the 3 plane reference system established on Part #2.Since the relationship to these datum reference planes is one of perpendicularity to the primary planes and distance/location from the secondary and tertiary planes, we choose a geometric tolerance capable of controlling angle and location. The most appropriate control is a position tolerance. A position tolerance must first be calculated. Since the shaft on Part #2 is “fixed” in place, the assembly of Part #1 and Part #2 is known as a “Fixed Fastener” assembly. The formula for a fixed fastener condition is:MMC Hole- MMC ShaftGeometric tolerance to be divided between shaft and hole99 = MMC HOLE- 97 = MMC SHAFT2 = Geometric Tolerance to be divided between Part #1 and Part #2Each part will receive 1 mm of position tolerance if the tolerance is equally divided. If one of the parts was determined to need more position tolerance than the other because of manufacturing difficulty, the 2 mm of geometric tolerance may be unequally divided. In this case, each part is determined to be equally hard to manufacture and will, therefore, be assigned 1 mm of position tolerance. If Part #1 had two holes and Part #2 had two shafts, each pattern of holes or shafts would still receive 1 mm of position tolerance. So, this method holds as true for a pattern of 100 holes and 100 shafts as it does in this situation of 1 hole and 1 shaft.Since these are mating features, the maximum material condition symbol will be used in the position control to allow a greater position tolerance as the hole is produced larger (and, therefore, mates easier) than its MMC of 99. Likewise, the maximum material condition symbol will be used in the position control to allow a greater position tolerance as the shaft is produced smaller (and, therefore, mates easier) than its MMC of 97.Step #4 completes the drawing changes and appears with